I'm very new to Mach3 and I have searched all over and looked in the support docs and the Turn manual for information on the tool adjust button to no avail. Its briefly mentioned in many places but nothing specific as to how you use it and what field you put the changes into.

I setup all the tools as per the instructions, and I understand all that. But when I setup the master tool or any tool the lathe and take a cut, I measure and see there is a difference of lets say +0.003 (part is larger that it should be) between where the software thinks the cut was and what it actually ended up with.

I assume tool adjust is for this purpose but which of the 10 fields do you put the change into. Wear.. offet, ? I'm in diameter mode so I would half that number to 0.0015, I got that. I'm on 066 and realize it has an issue with some turn functions. I will be reverting to 064 or 057.

The other question is when I make a change to the master does it make the change to all tools or do I change each individually.I'm thinking more of changing on the fly to dial in the part being turned.

For all the new guys I found that there are a few ways to do tool cut adjustments on the fly. The easiest being "Tool Adjust" and enter the desired correction into the wear field off either X or ZThis is for lathe front tool post in diameter mode.

After you setup your tooling and make a few test runs, you can enter the needed adjustment or as your turning a run of parts and periodically need to compensate for tool wear or other anomalies on the X or Z axis. Enter the whole number of the difference between the cut and measurement, if it's 0.005 larger in diameter you need to enter -0.005. if its 0.005 to small enter +0.005. + brings the tool out toward you and - brings it in away from you. Z is the same thing. Anything to the right of Z0.0 will be + and anything to the left of Z0.0 is -

The entries for a tool in tool table are added up for in each tool to give you the offset or position of the control point. Using tool wear does not change the base offset for any particular tool it just adds to or takes from that tool. So changing the #1 master tool by using X Wear does not change how you set it up in tool table as Z 0.000 X0.0000 and does not change the relationships between master and the other tools, that remains unchanged. If you enter for the master #1 tool 0.0015 in X wear you will see the Z0.000 X 0.000 stay the same and X wear as 0.00075 and it will cut the the part larger by 0.0015.

You just need to remember you have a wear entry in the table when setting up for another job or changing the inserts

Note the following:- The master tool sets the basis for all the other tool offsets. I use tool #1 for the master tool and it has no offsets just like Tool 0 which has no offsets and you can't change Tool 0. One can simply say that all tools relate to the master tool and all tools relate to each other.- All tool X offsets are in terms of radii in the tool table. - Do not mix front and rear post in the tool table.- The X & Z wear offset can be used to adjust the work offset. Inserts have tolerances, and frankly I just rather re- touch off the tool with the new insert. You can call out the same tool but use the offset of another tool.- Once the tool table is populated you should not need to change anything unless there is wear,breakage , etc. - Any touch off method and use of a tool is only as good as YOUR LATHE SYSTEM.- There are a number of ways to populate the tool table. Making a cut and and using the machine value will be most accurate for most. - Consider using Radius mode and machine coordinates when populating the tool table.- Also always recheck / confirm tool offsets & adjustments as one does make mistakes.

I don't use the generic screen set and use a custom screen set to probe for tool offsets and populate the table. Frankly repeatablity of touch off is +- 0.0002" and that is as good as actualy turning down and measuring and also is much quicker.

I do have a question........What "Tool Adjust" button are you taking about? There is no button like that in the generic screen set.

All good info, You are correct the better you setup your tool the less you have out of tolerance issues, but being a novice I'm prone to beginner errors and bad methods just because I don't know better.

I'm on 062 now and in the lathe > Auto > Cycle , there is a button just under the code window that says "Tool Adjust". In some documentation it mentions it but only in one sentence, basically this is where you do that adjustment but no reference as to which dro or how to enter i.e... diameter, radius, half number or full number.

I wanted to use it for making adjustments on the fly as I run a job of 100 or so items. I setup the job and tooling as per the manual then run a few and make the adjustment and run a few more an see where it is, if it's good I check every 10 - 15 and adjust if needed. but as I said its mainly due to me being a nube on CNC and most likely not having setup correctly. I did find some backlash issues that I corrected that also contributed to the variances.

Thoroco,Thanks for button info. TOOL TABLE button on the first screen is the same as Tool Adjustment button in the cycle screen and they are just a button to take you to the page used for setting up your lathe tools.

1.All tool X offsets are in terms of radii in the tool table. Diameter Mode - the X axis would only move 1/2 of the distance of the value. Radius Mode - " " the value 2.Consider using Radius mode and machine coordinates when populating the tool table. When in Machine Coordinates the axis moves are absolute and the actual x axis moves will be in terms of radii. --------------------------------------For adjusting or manualy putting the X offset into the tool table:

If in Diameter Mode, then input the offset in terms of diameter, open the tool tableand you will see that it is 1/2 of the value you input into the X offset DRO.

If in Radius Mode, then input the desired X offset , open the tool tableand you will see that it is the value you input into the X offset DRO .

The above also applies to X wear.--------------------------------------Yes it can get confusing. So lets add to the confusion.........try this!In Radius Mode put a value into the X offset and X wear. Open the tool table and check that the inputs are as input, click Apply and Ok. Now change the mode from Radius to Diameter ( Config> Ports & Pins>Turn Options> tick Diameter for x mode) ( BTW, you can't change x mode any other way ). What occured in the tool set up screen?

---------------------------------------

You can setup anyway you want. Simply here is what I do:1. Tool table is populated / complete and done. 2. Locate lathe center X =0 ( I probe for it with the master tool)3. Define a location such that Machine Coordinate 0,0=Home / referenced location 0,0= the tool change location, all of which is far enough away from the stock for all the tools. 4. Locate the part / stock from home. ( I probe it with Tool #0) G54 work offset is created.5. Home the axes, insert first tool to be used, run the program

I kind of figure out what your saying above the more I looked into it. As a beginner we tend to forget that if your move the tool in .005 your actually cutting .010 off the part on a manual lathe. Here the CnC software takes into consideration the Mode your in and compensates.

If I setup all 12 tools I use as per the manual and go to setup a work piece that uses only 3 tools. Do I need to set it up off of the master each time or can I setup off a tool it will be turned with.

Example . I use a general turning tool Angle Right Diamond shaped as #5 tool and a Drill as #10 and a cutoff as #3. My operation is drill a hole with #10, then turn a chamfer on the end and turn down the OD with #5, then cut off with #3. Its all in the code to do tool changes and it works as its supposed to but I always setup off of #1 even if I'm not using #1. Can I setup off of any tool I'm actually using or is it best to setup from the master.

Setting up a drill chucks. If I set up a drill chuck I need to make sure it's aligned with X0.0 and not on an angle so it drills straight and does not taper the hole or worse bind and snap a drill. what is the recommended way to square the tool post with the lathe chuck? What I have been doing is put a piece of drill rod in the chuck loosen the QCTP and the move the drill chuck onto the drill rod and adjust and tighten it all down, Then go and setup all the tool starting at master and working my way to #10 drill #11 drill an #13 boring bar. Is there an easier way to set up drill chucks?

Study what is written in a text file called MachTurn which can be found in the Mach3 folder you installled Mach. The file file dates back to 2006 but represents the thinking on how the generic screen set is used and a way to set things up.

I echo what I posted before and added in quotations:

One can simply say that all tools relate to the master tool and all tools relate to each other "including the master tool".

Do I need to set it up off of the master each time or can I setup off a tool it will be turned with.

Can I setup off of any tool I'm actually using or is it best to setup from the master.

I personaly always use the master tool but you can use any tool provided the tool table work offsets are correct. Also remember to make sure that the tool # DRO shows the tool to be used!!! What you do is dependent on what method you are using ie; if the tool is not used for actual machining and your going to use the screen to machine and use the inputs to define the location of the work then you need to use the proper tool.

I hope you are not getting confused.

Quote

Is there an easier way to set up drill chucks?

A number of ways to do. You can try this or a variation of it. If a reference piece has an accurate hole on the center ( ie; reamed hole for the size of drill) and if reference piece is truely on center then when you move the drill into the the reamed hole it will enter without any movement. Need to look at it under magnification. That is how I check the small size drills #60 to #80. Adjust tool holder / chuck until that happens. I probe mine and they are usualy spot on, but....... the micro drills will break in a heart beat ( especialy carbide ones) if not set properly.

Must say that everything one does is only as good as the "Lathe System" and how meticulous they are in setup.

Must note that I have use Albrecht drill chuck's and lucky to have a set.